<!DOCTYPE html>
<html>
<head>
<title>DEVELOPER INFO</title>
<link rel="stylesheet" type="text/css" href="xschem_man.css" />
<style type="text/css">
/* Local styling goes here */
p{padding: 15px  30px 10px;}

</style>

</head>
<body>

<!-- start of slide -->
<div class="content">   
<!-- navigation buttons -->
<a href="graphs.html" class="prev">PREV</a>
<a href="xschem_man.html" class="home">UP</a>
<a href="xschem_remote.html" class="next">NEXT</a>
 <!-- slide title -->
 <h1>DEVELOPER INFO</h1><br>
 <h3>GENERAL INFORMATION</h3>
 <p>
  XSCHEM uses layers for its graphics, each layer is a logical entity defining graphic attributes 
  like color and fill style.  There are very few graphical primitive objects:
 </p>
 <ol>
  <li>Lines</li>
  <li>Rectangles</li>
  <li>Open / close Polygons</li>
  <li> Arcs / Circles</li>
  <li>Text</li>
 </ol>
 <p>
  These primitive objects can be drawn on any layer. XSCHEM number of layers can be defined at compile
  time, however there are some predefiend layers (from 0 to 5) that have specific functions:
 </p>
 <ol start="0">
 <li>Background color</li>
 <li>Wire color (nets)</li>
 <li>Selection color / grid</li>
 <li>Text color</li>
 <li>Symbol drawing color</li>
 <li>Pin color</li>
 <li>General purpose</li>
 <li>General purpose</li>
 <li>General purpose</li>
 </ol>
 <p style="margin-left:30px;">
 ....
 </p>
 <ol start="20">
 <li>General purpose</li>
 <li>General purpose</li>
 </ol>
 <p>
  Although any layer can be used for drawing it is strongly advisable to avoid the
  background color and the selection color to avoid confusion.
  Drawing begins by painting the background (layer 0), then drawing the grid (layer 1) 
  then drawing wires (nets) on layer 2, then all graphical objects (lines, rectangles, polygons)
  starting form layer 0 to the last defined layer.
 </p>
 <h3>SYMBOLS</h3>
 <p>
  There is a primitive object called symbol. Symbols are just a group of primitive graphic objects 
  (lines, polygons, rectangles, text) that can be shown as a single atomic entity.
  Once created a symbol can be placed in a schematic. The instantiation of a symbol is called 'component'.
 </p>
 <img src="building_symbol_03.png">
 <p>
  The above picture shows a resistor symbol, built drawing some lines on layer 4 (green),
  some pins on layer 5 (red) and some text.
  Symbols once created are stored in libraries (library is just a UNIX directory known to XSCHEM)
  and can be placed like just any other primitive object multiple times in a schematic window
  with different orientations.
 </p>
 <img src="developer_info_01.png">
 <h3>WIRES</h3>
 <p>
  Another special primitive object in XSCHEM is 'Wire', Graphically it is drawn as a line on layer 1 (wires).
  Wires are drawn only on this layer, they are treated differently by XSCHEM since they carry electrical 
  information. Electrical connection between components is done by drawing a connecting wire.
 </p>
 <p class="important">
  Since wires are used to build the circuit connectivity it is best to avoid drawing lines on layer 1 
  to avoid confusion, since they would appear like wires, but ignored completely for electrical connectivity.
 </p>
 <h3>PROPERTIES </h3>
 <p>
  All XSCHEM objects (wires, lines, rectangles, polygons, text, symbol instance aka component)
  have a property string attached. Any text can be present in a property string, however 
  in most cases the property string is organized as a set of <kbd>key=value</kbd> pairs separated by white space.
  In addition to object properties the schematic or symbol view has global properties attached. 
  There is one global property defined per netlisting mode (currently SPICE, VHDL, Verilog, tEDAx) and one additional global property
  for symbols (containing the netlisting rules usually).
  See the <a href="xschem_properties.html">XSCHEM properties</a> section of the manual for more info.
 </p>
 <h3>COORDINATE SYSTEM</h3>
 <p>
  XSCHEM coordinates are stored as double precision floating point numbers, axis orientation is the same as Xorg
  default coordinate orientation: 
 </p>
 <img src="developer_info_02.png">
 <p>
  When drawing objecs in XSCHEM coordinates are snapped to a multiple of 10.0 coordinate units,
  so all drawn objects are easily aligned.
  The snap level can be changed to any value by the user to allow drawing small objects if desired.
  Grid points are shown at multiples of 20.0 coordinate units, by default.
 </p>
 <h2>XSCHEM FILE FORMAT SPECIFICATION</h2>
 <p>
  XSCHEM schematics and symbols are stored in .sch and .sym files respectively. The two file formats are identical, with the
  exception that symbol (.sym) files usually do not contain wires and component instantiations (although they can).
 </p>
 <p>
  every schematic/symbol object has a corresponding record in the file.
  A single character at the beginning of a line, separated by white space from subsequent fields marks the type of object:
 </p>
 <ul>
  <li><kbd>v</kbd> : XSCHEM Version string
  <li><kbd>S</kbd> : Global property associated to the .sch file for SPICE netlisting</li>
  <li><kbd>V</kbd> : Global property associated to the .sch file for VERILOG netlisting</li>
  <li><kbd>G</kbd> : Global property associated to the .sch file for VHDL netlisting OR
                     Global property associated to the .sym file for netlisting (in 1,2 file 
                     format <kbd>K</kbd> is used, although backward compatibility is guaranteed)</li>
  <li><kbd>E</kbd> : Global property associated to the .sch file for tEDAx netlisting</li>
  <li><kbd>K</kbd> : Global property associated to the .sch/sym file for netlisting.<br>
                     For schematic it is used if instantiated as a component (file format 1.2 and newer) </li> 
  <li><kbd>L</kbd> : Line </li>
  <li><kbd>B</kbd> : Rectangle </li>
  <li><kbd>P</kbd> : Open / Closed polygon </li>
  <li><kbd>A</kbd> : Arc / Circle </li>
  <li><kbd>T</kbd> : Text </li>
  <li><kbd>N</kbd> : Wire, used to connect together components (only in .sch files) </li>
  <li><kbd>C</kbd> : Component instance in a schematic (only in .sch files) </li>
  <li><kbd>[</kbd> : Start of a symbol embedding, the symbol refers to the immediately preceding component instance.
                     This tag must immediately follow a component instance (<kbd>C</kbd>). 
                     See the example here under. A component symbol is embedded into the schematic file when saving
                     if the <kbd>embed=true</kbd> attribute is set on one of the component instances.
                     Only one copy of the embedded symbol is saved into the schematic and all components
                     referring to this symbol will use the embedded definition.
                     When a component has an embedded symbol definition immediately following, a <kbd>embed=true</kbd> is
                     added to the component property string if not already present.
                     </li><br>
  
     <pre class="code">
C {TECHLIB/PCH} 620 -810 0 0 {name=x5 model=PCHLV w=4 l=0.09  m=1 embed=true}
[
v {xschem version=2.9.7 file_version=1.2}
G {}
K {type=pmos
format="@name @pinlist @model w=@w l=@l m=@m"
verilog_format="@verilog_gate #(@del ) @name ( @@d , @@s , @@g );"
template=" name=x1 verilog_gate=pmos del=50,50,50 model=PCH w=0.68 l=0.07 m=1 "
generic_type="model=string"
}
V {}
S {}
E {}
L 4 5 20 20 20 {}
L 4 20 20 20 30 {}
L 4 5 -20 20 -20 {}
L 4 20 -30 20 -20 {}
L 4 -20 0 -10 0 {}
L 4 5 -27.5 5 27.5 {11}
L 4 5 -5 10 0 {}
L 4 5 5 10 0 {}
L 4 10 0 20 0 {}
L 18 -2.5 -15 -2.5 15 {}
B 5 17.5 27.5 22.5 32.5 {name=d dir=inout}
B 5 -22.5 -2.5 -17.5 2.5 {name=g dir=in}
B 5 17.5 -32.5 22.5 -27.5 {name=s dir=inout}
B 5 17.5 -2.5 22.5 2.5 {name=b dir=in}
A 4 -6.25 0 3.75 270 360 {}
T {@w/@l*@m} 7.5 -17.5 0 0 0.2 0.2 {}
T {@name} 7.5 6.25 0 0 0.2 0.2 {999}
T {@model} 2.5 -27.5 0 1 0.2 0.2 {layer=8}
T {D} 25 17.5 0 0 0.15 0.15 {layer=13}
T {NF=@nf} -5 -15 0 1 0.15 0.15 {}
]
</pre><br>
  <li><kbd>]</kbd> : End of an embedded symbol. </li>
 </ul>
 <p>
  the object tag in column 1 is followed by space separated fields that completely define the corresponding object.
 </p>
 <h3>VERSION STRING</h3>
 <p>
  Example: <kbd><br>
v {xschem version=2.9.7 file_version=1.2}</kbd>
 </p>
 <p>
  Two attributes are defined, the xschem version and the file format version.
  Current file format version is 1.2. This string is guaranteed to be the first one in XSCHEM .sch and .sym files.

  A comment can be added (by manually editing the xschem schematic or symbol file) as shown below:
 </p>
 <pre class="code">
v {xschem version=3.1.0 file_version=1.2 
* Copyright 2022 Stefan Frederik Schippers
* 
* Licensed under the Apache License, Version 2.0 (the "License");
* you may not use this file except in compliance with the License.
* You may obtain a copy of the License at
*
*     https://www.apache.org/licenses/LICENSE-2.0
*
* Unless required by applicable law or agreed to in writing, software
* distributed under the License is distributed on an "AS IS" BASIS,
* WITHOUT WARRANTIES OR CONDITIONS OF ANY KIND, either express or implied.
* See the License for the specific language governing permissions and
* limitations under the License.
}
</pre>
 <h3>GLOBAL SCHEMATIC/SYMBOL PROPERTIES</h3>
 <p>
  Example:<kbd><br>
K {type=regulator<br>
format="x@name @pinlist r@symname"<br>
verilog_format="assign @#2 = @#0 ;"<br>
tedax_format="footprint @name @footprint<br>
device @name @symname"<br>
template="name=U1 footprint=TO220"}</kbd>
 </p>
 <p>
  Global properties define a property string bound to the parent schematic/symbol file,
  there is one global property record per netlisting mode, 
  currently SPICE, VHDL, Verilog, tEDAx.<br>
  In addition (only in file_format 1.2 and newer) for schematics and symbols there is a global attribute ('K') 
  that defines how to netlist the schematic/symbol if placed as a 
  symbol into another parent schematic (should be set in the same way as the 'G' global attribute for symbols
  in pre-1.2 file format).
  Normally only 'G' ('K' in 1.2 file format) type property strings are used for symbols and define attributes
  telling netlisters what to do with the symbol, while global property 
  strings in schematic files corresponding to the active netlisting mode of XSCHEM are
  copied verbatim to the netlist.<br>
  the object tag (S, V, G, E, K) is followed by the property string enclosed in curly braces 
  (<kbd>{...}</kbd>). This allows strings to contain any white space and newlines.
  Curly braces if present in the string are automatically escaped with the '\' character
  by XSCHEM when saving data.<br>
  Example of the 4 property string records for a schematic file:<kbd><br>
G {} <br>
V {assign #1500 LDOUT = LDIN +1;<br>
} <br>
E {}<br>
S {}</kbd><br>
in this case only the verilog-related global property has some definition. This is Verilog code that is copied into the output netlist.
 </p>

 <p class="important">
  Attribute strings for all Xschem objects are enclosed in curly braces. 
  This allows attributes to span multiple lines.
  This component instance:<br>
   <kbd>C {capa.sym} 890 -160 0 0 {name=C4 m=1 value=10u device="tantalium capacitor"}</kbd><br>
  and this one:<br>
   <kbd>C {capa.sym} 890 -160 0 0 {name=C4<br>
m=1 value=10u<br>
device="tantalium capacitor"<br>
}</kbd><br>
  are perfectly equivalent.
 </p>

 <a id="textobj"><h3>TEXT OBJECT</h3></a>
 <p>
  Example: <kbd>T {3 of 4 NANDS of a 74ls00} 500 -580 0 0 0.4 0.4 {font=Monospace layer=4}</kbd><br>
  This line defines a text object, the first field after the type tag is the displayed text,
  followed by X and Y coordinates,rotation, mirror, 
  horizontal and vertical text size and finally a property string defining some text attributes.
  <ul>
   <li>The displayed text is enclosed in curly braces (<kbd>{...}</kbd>) to allow white space. Literal curly braces 
   must be escaped if present in the saved string. XSCHEM will automatically add the escapes where needed on save.</li>
   <li>X ad Y coordinates are saved and retrieved as double precision floating point numbers.</li>
   <li>Rotation and mirror are integers (range [0:3], [0:1] respectively) that define the orientation 
   of text objects. Using rotation and mirror text can be aligned to any corner of its bounding box, so there are 4 different 
   alignments for vertical text and 4 different alignments for horizontal text. Below picture shows how text is displayed
   with respect to its anchor point.
   <img src="developer_info_03.png"></li>
   <li> text X and Y sizes are stored as floating point numbers.</li>
   <li> Finally a property string is available to attach attributes to the text object.
        Currently the following attributes are predefined for text objects:<br><br>
        <ul>
         <li><kbd>font</kbd> Name of font to be used (ex: font=Arial)</li>
         <li><kbd>layer</kbd> Number of layer to use for drawing (as in Xschem Layers menu)</li>
         <li><kbd>hcenter</kbd> If set to <kbd>true</kbd> horizontal center text</li>
         <li><kbd>vcenter</kbd> If set to <kbd>true</kbd> vertical center text</li>
         <li><kbd>weight</kbd> If set to <kbd>bold</kbd> use bold style</li>
         <li><kbd>slant</kbd> If set to <kbd> italic</kbd> or <kbd>oblique</kbd> use that style for text</li>
         <li><kbd>hide</kbd> If set to <kbd>true</kbd> text will be hidden unless <kbd>View-&gt;Show hidden texts</kbd>
           is enabled<br>
           If <kbd>hide=instance</kbd> is given the text will be invisible in placed instances of the 
           symbol, but visible when descending into the symbol.</li>
        </ul>
   </li>
  </ul> 
 </p>
 <h3>WIRE OBJECT</h3>
 <p>
  Example: <kbd>N 890 -130 890 -110 {lab=ANALOG_GND}</kbd><br>
  The net 'N' tag is followed by the end point coordinates x1,y1 - x2,y2.
  (stored and read as double precision numbers) and a property string, used in this case to name the net.
  In most cases you don't need to specify attributes for nets (one exception is the <kbd>bus</kbd> attribute)
  as the <kbd>lab</kbd> attribute is set by xschem when creating a netlist or more generally when
  building the connectivity.
  This means that almost always nets in a xschem schematic are set as in following example:<br>
   <kbd>N 890 -130 890 -110 {}</kbd><br>
  Xschem schematic files store only geometrical data and attributes of the graphic primitives, 
  the connectivity and the logical network is obtained by xschem. 
 </p>
 <h3>LINE OBJECT</h3>
 <p>
  Example: <kbd>L 4 -50 20 50 20 {This is a line on layer 4}</kbd><br>
  The line 'L' tag is followed by an integer specifying the graphic layer
 followed by the x1,y1 - x2,y2 coordinates of the line and a property string.
 </p>
 <h3>RECTANGLE OBJECT</h3>
 <p>
  Example: <kbd>B 5 -62.5 -2.5 -57.5 2.5 {name=IN dir=in pinnumber=1}</kbd><br>
  The 'Box' 'B' tag is followed by an integer specifying the graphic layer followed
  by the x1,y1 - x2,y2 coordinates of the rectangle
  and a final property string. This example defines a symbol pin.
 </p>
 <h3>OPEN / CLOSED POLYGON OBJECT</h3>
 <p>
  Example: <kbd>P 3 5 2450 -210 2460 -170 2500 -170 2510 -210 2450 -210 {}</kbd><br>
  the Polygon 'P' tag is followed by an integer specifying the layer number,
  followed by the number of points (integer), 
  the x,y coordinates of the polygon points and the property string (empty in this example).
  If the last point is coincident to the first point a closed polygon is drawn.
  A 'fill=true' arribute may be given to fill a closed polygon, in this case a polygon line looks like:<br>
  <kbd>P 3 5 2450 -210 2460 -170 2500 -170 2510 -210 2450 -210 {fill=true}</kbd><br>
 </p>
 <h3>ARC OBJECT</h3>
 <p>
  Example: <kbd>A 3 450 -210 120 45 225 {}</kbd><br>
  The Arc 'A' tag is followed by an integer specifying the layer number, followed by the arc x, y center coordinates,
  the arc radius, the start angle (measured counterclockwise from the three o'clock direction), the arc sweep angle
  (measured counterclockwise from the start angle) and the property string (empty in this example).
  Angles are measured in degrees.<br>
  <img src="developer_info_07.png">
 </p>
 <h3>COMPONENT INSTANCE</h3>
 <p>
  Example: <kbd>C {capa.sym} 890 -160 0 0 {name=C4 m=1 value=10u device="tantalium capacitor"}</kbd><br>
  Format: <kbd>C {&lt;symbol reference&gt;} &lt;X coord&gt; &lt;Y coord&gt; &lt;rotation&gt;
          &lt;flip&gt; {&lt;attributes&gt;}</kbd><br>
  The component instance tag C is followed by a string specifying <kbd>library/symbol</kbd> or only <kbd>symbol</kbd> 
  (see <a href="tutorial_xschem_libraries.html">This tutorial about symbol references</a>)
  followed by the x,y coordinates, rotation (integer range [0:3]), 
  mirror (integer range [0:1]), and a property string defining various attributes
  including the mandatory <kbd>name=...</kbd> attribute.<br>
  Orientation and mirror meanings are as follows:<br>
  <img src="developer_info_04.png">
 </p>
 <h3>EXAMPLE OF A COMPLETE SYMBOL FILE (7805.sym)</h3><br>
 <pre class="code">
G {}
K {type=regulator
format="x@name @pinlist r@symname"
verilog_format="assign @#2 = @#0 ;"
tedax_format="footprint @name @footprint
device @name @symname"
template="name=U1 footprint=TO220"}
V {}
S {}
E {}
L 4 -60 0 -50 0 {}
L 4 50 0 60 0 {}
L 4 -50 -20 50 -20 {}
L 4 50 -20 50 20 {}
L 4 -50 20 50 20 {}
L 4 -50 -20 -50 20 {}
L 4 0 20 0 30 {}
B 5 -62.5 -2.5 -57.5 2.5 {name=IN dir=in pinnumber=1}
B 5 -2.5 27.5 2.5 32.5 {name=GND dir=inout pinnumber=2}
B 5 57.5 -2.5 62.5 2.5 {name=OUT dir=out pinnumber=3}
T {@name} -17.5 -15 0 0 0.2 0.2 {}
T {@symname} -17.5 0 0 0 0.2 0.2 {}
T {@#0:pinnumber} -47.5 -2.5 0 0 0.12 0.12 {}
T {@#1:pinnumber} -2.5 12.5 0 0 0.12 0.12 {}
T {@#2:pinnumber} 47.5 -2.5 0 1 0.12 0.12 {}
 </pre>
 <img src="developer_info_05.png"><br>
 <br>
 <h3>EXAMPLE OF A COMPLETE SCHEMATIC FILE (pcb_test1.sch)</h3><br>
 <pre class="code">
G {}
K {}
V {}
S {}
E {}
B 20 270 -550 860 -290 {}
T {3 of 4 NANDS of a 74ls00} 500 -580 0 0 0.4 0.4 {}
T {EXPERIMENTAL schematic for generating a tEDAx netlist
1) set netlist mode to 'tEDAx' (Options menu -> tEDAx netlist)
2) press 'Netlist' button on the right
3) resulting netlist is in pcb_test1.tdx } 240 -730 0 0 0.5 0.5 {}
N 230 -330 300 -330 {lab=INPUT_B}
N 230 -370 300 -370 {lab=INPUT_A}
N 680 -420 750 -420 {lab=B}
N 680 -460 750 -460 {lab=A}
N 400 -350 440 -350 {lab=B}
N 850 -440 890 -440 {lab=OUTPUT_Y}
N 230 -440 300 -440 {lab=INPUT_F}
N 230 -480 300 -480 {lab=INPUT_E}
N 400 -460 440 -460 {lab=A}
N 550 -190 670 -190 {lab=VCCFILT}
N 590 -130 590 -110 {lab=ANALOG_GND}
N 790 -190 940 -190 {lab=VCC5}
N 890 -130 890 -110 {lab=ANALOG_GND}
N 730 -110 890 -110 {lab=ANALOG_GND}
N 730 -160 730 -110 {lab=ANALOG_GND}
N 590 -110 730 -110 {lab=ANALOG_GND}
N 440 -460 680 -460 {lab=A}
N 500 -420 680 -420 {lab=B}
N 500 -420 500 -350 {lab=B}
N 440 -350 500 -350 {lab=B}
C {title.sym} 160 -30 0 0 {name=l2 author="Stefan"}
C {74ls00.sym} 340 -350 0 0 {name=U1:2  risedel=100 falldel=200}
C {74ls00.sym} 790 -440 0 0 {name=U1:1  risedel=100 falldel=200}
C {lab_pin.sym} 890 -440 0 1 {name=p0 lab=OUTPUT_Y}
C {capa.sym} 590 -160 0 0 {name=C0 m=1 value=100u device="electrolitic capacitor"}
C {74ls00.sym} 340 -460 0 0 {name=U1:4 risedel=100 falldel=200 power=VCC5
url="http://www.engrcs.com/components/74LS00.pdf".sym}
C {LM7805.pdf"}
C {lab_pin.sym} 490 -190 0 0 {name=p20 lab=VCC12}
C {lab_pin.sym} 940 -190 0 1 {name=p22 lab=VCC5}
C {lab_pin.sym} 590 -110 0 0 {name=p23 lab=ANALOG_GND}
C {capa.sym} 890 -160 0 0 {name=C4 m=1 value=10u device="tantalium capacitor"}
C {res.sym} 520 -190 1 0 {name=R0 m=1 value=4.7 device="carbon resistor"}
C {lab_wire.sym} 620 -460 0 0 {name=l3 lab=A}
C {lab_wire.sym} 620 -420 0 0 {name=l0 lab=B}
C {lab_wire.sym} 650 -190 0 0 {name=l1 lab=VCCFILT}
C {connector.sym} 230 -370 0 0 {name=CONN1 lab=INPUT_A verilog_type=reg}
C {connector.sym} 230 -330 0 0 {name=CONN2 lab=INPUT_B verilog_type=reg}
C {connector.sym} 240 -190 0 0 { name=CONN3 lab=OUTPUT_Y }
C {connector.sym} 230 -480 0 0 {name=CONN6 lab=INPUT_E verilog_type=reg}
C {connector.sym} 230 -440 0 0 {name=CONN8 lab=INPUT_F verilog_type=reg}
C {connector.sym} 240 -160 0 0 { name=CONN9 lab=VCC12 }
C {connector.sym} 240 -130 0 0 { name=CONN14 lab=ANALOG_GND  verilog_type=reg}
C {connector.sym} 240 -100 0 0 { name=CONN15 lab=GND  verilog_type=reg}
C {code.sym} 1030 -280 0 0 {name=TESTBENCH_CODE only_toplevel=false value="initial begin
  $dumpfile(\\"dumpfile.vcd\\");
  $dumpvars;
  INPUT_E=0;
  INPUT_F=0;
  INPUT_A=0;
  INPUT_B=0;
  ANALOG_GND=0;
  #10000;
  INPUT_A=1;
  INPUT_B=1;
  #10000;
  INPUT_E=1;
  INPUT_F=1;
  #10000;
  INPUT_F=0;
  #10000;
  INPUT_B=0;
  #10000;
  $finish;
end

assign VCC12=1;

"}
C {verilog_timescale.sym} 1050 -100 0 0 {name=s1 timestep="1ns" precision="1ns" }
 </pre>
 <img src="developer_info_06.png"><br>
 <br>
 <h1>XSCHEM <a id="cmdref">COMMAND REFERENCE</a> DOCUMENTATION</h1><br>
 <p>
   The following are xschem specific tcl commands.
   All commands are prefixed by the <kbd>xschem</kbd> keyword.
   <br>
   Example:
 </p>
 <pre class="code">
     <strong>xschem</strong> getprop instance x3 OFFSET </pre>
 <br>
 <ul> <!-- Following list items generated in xschem src dir with: 
             ./extract_scheduler_cmd_help.awk scheduler.c > ~/xxx 
           Include ~/xxx here between <ul> and </ul>
        -->



































































   <li><kbd>       abort_operation</kbd></li><pre>
   Resets UI state, unselect all and abort any pending operation </pre>
   <li><kbd>       add_symbol_pin</kbd></li><pre>
   Start a GUI placement of a symbol pin </pre>
   <li><kbd>       add_graph</kbd></li><pre>
   Start a GUI placement of a graph object </pre>
   <li><kbd>       add_png</kbd></li><pre>
   Ask user to choose a png file and start a GUI placement of the image </pre>
   <li><kbd>       align</kbd></li><pre>
   Align currently selected objects to current snap setting </pre>
   <li><kbd>       annotate_op [raw_file] [level]</kbd></li><pre>
   Annotate operating point data into current schematic. 
   use &lt;schematic name&gt;.raw or use supplied argument as raw file to open
   look for operating point data and annotate voltages/currents into schematic.
   The optional 'level' integer specifies the hierarchy level the raw file refers to.
   This is necessary if annotate_op is called from a sub schematic at a hierarchy
   level &gt; 0 but simulation was done at top level (hierarchy 0, for example)</pre>
   <li><kbd>       arc</kbd></li><pre>
   Start a GUI placement of an arc.
   User should click 3 unaligned points to define the arc </pre>
   <li><kbd>       attach_labels</kbd></li><pre>
   Attach net labels to selected component(s) instance(s) </pre>
   <li><kbd>       bbox begin|end</kbd></li><pre>
   Start/end bounding box calculation: parameter is either 'begin' or 'end' </pre>
   <li><kbd>       break_wires [remove] </kbd></li><pre>
   Break wires at selected instance pins
   if '1' is given as 'remove' parameter broken wires that are
   all inside selected instances will be deleted </pre>
   <li><kbd>       build_colors</kbd></li><pre>
   Rebuild color palette using values of tcl vars dim_value and dim_bg </pre>
   <li><kbd>       callback winpath event mx my key button aux state</kbd></li><pre>
   Invoke the callback event dispatcher with a software event </pre>
   <li><kbd>       case_insensitive 1|0</kbd></li><pre>
   Set case insensitive symbol lookup. Use only on case insensitive filesystems </pre>
   <li><kbd>       change_elem_order n</kbd></li><pre>
   set selected object (instance, wire, line, rect, ...) to
   position 'n' in its respective array </pre>
   <li><kbd>       check_symbols</kbd></li><pre>
   List all used symbols in current schematic and warn if some symbol is newer </pre>
   <li><kbd>       check_unique_names [1|0]</kbd></li><pre>
   Check if all instances have a unique refdes (name attribute in xschem), 
   highlight such instances. If second parameter is '1' rename duplicates </pre>
   <li><kbd>       circle</kbd></li><pre>
   Start a GUI placement of a circle.
   User should click 3 unaligned points to define the circle </pre>
   <li><kbd>       clear [force] [symbol|schematic]</kbd></li><pre>
   Clear current schematic window. Resets hierarchy level. Remove symbols
   the 'force' parameter will not ask to save existing modified schematic.
   the 'schematic' or 'symbol' parameter specifies to default to a schematic
   or symbol window (default: schematic) </pre>
   <li><kbd>       clear_drawing</kbd></li><pre>
   Clears drawing but does not purge symbols </pre>
   <li><kbd>       color_dim value</kbd></li><pre>
   Dim colors or brite colors depending on value parameter: -5 &lt;= value &lt;= 5 </pre>
   <li><kbd>       compare_schematics [sch_file]</kbd></li><pre>
   Compare currently loaded schematic with another 'sch_file' schematic.
   if no file is given prompt user to choose one </pre>
   <li><kbd>       connected_nets [0|1|2|3]</kbd></li><pre>
   Select nets/labels  connected to currently selected instance
   if '1' argument is given, stop at wire junctions
   if '2' argument is given select only wires directly
   attached to selected instance/net
   if '3' argument is given combine '1' and '2' </pre>
   <li><kbd>       copy</kbd></li><pre>
   Copy selection to clipboard </pre>
   <li><kbd>       copy_hierarchy to from</kbd></li><pre>
   Copy hierarchy info from tab/window "from" to tab/window "to"
   Example: xschem copy_hierarchy .drw .x1.drw </pre>
   <li><kbd>       copy_objects [deltax deltay [rot flip]]</kbd></li><pre>
   if deltax and deltay (and optionally rot and flip) are given copy selection
   to specified offset, otherwise start a GUI copy operation </pre>
   <li><kbd>       count_items string separator quoting_chars</kbd></li><pre>
   Debug command </pre>
   <li><kbd>       create_plot_cmd</kbd></li><pre>
   Create an xplot file in netlist/simulation directory with
   the list of highlighted nodes in a format the selected waveform
   viewer understands (bespice, gaw, ngspice) </pre>
   <li><kbd>       cut</kbd></li><pre>
   Cut selection to clipboard </pre>
   <li><kbd>       debug n</kbd></li><pre>
   Set xschem in debug mode.'n' is the debug level 
   (0=no debug). Higher levels yield more debug info.</pre>
   <li><kbd>       delete</kbd></li><pre>
   Delete selection </pre>
   <li><kbd>       delete_files</kbd></li><pre>
   Bring up a file selector the user can use to delete files </pre>
   <li><kbd>       descend [n]</kbd></li><pre>
   Descend into selected component instance. Optional number 'n' specifies the 
   instance number to descend into for vector instances (default: 0). </pre>
   <li><kbd>       descend_symbol</kbd></li><pre>
   Descend into the symbol view of selected component instance </pre>
   <li><kbd>       destroy_all [force]</kbd></li><pre>
   Close all additional windows/.tabs. If 'force' is given do not ask for
   confirmation for changed schematics
   Returns the remaining # of windows/tabs in addition to main window/tab </pre>
   <li><kbd>       display_hilights [nets|instances]</kbd></li><pre>
   Print a list of highlighted objects (nets, net labels/pins, instances)
   if 'instances' is specified list only instance highlights
   if 'nets' is specified list only net highlights </pre>
   <li><kbd>       draw_graph [n] [flags]</kbd></li><pre>
   Redraw graph rectangle number 'n'.
   If the optional 'flags' integer is given it will be used as the 
   flags bitmask to use while drawing (can be used to restrict what to redraw) </pre>
   <li><kbd>       edit_file</kbd></li><pre>
   Edit xschem file of current schematic if nothing is selected.
   Edit .sym file if a component is selected. </pre>
   <li><kbd>       edit_prop</kbd></li><pre>
   Edit global schematic/symbol attributes or attributes
   of currently selected instances </pre>
   <li><kbd>       edit_vi_prop</kbd></li><pre>
   Edit global schematic/symbol attributes or
   attributes of currently selected instances
   using a text editor (defined in tcl 'editor' variable) </pre>
   <li><kbd>       embed_rawfile raw_file</kbd></li><pre>
   Embed base 64 encoded 'raw_file' into currently
   selected element as a 'spice_data'
   attribute. </pre>
   <li><kbd>       enable_layers</kbd></li><pre>
   Enable/disable layers depending on tcl array variable enable_layer() </pre>
   <li><kbd>       escape_chars source</kbd></li><pre>
   escape tcl special characters with backslash </pre>
   <li><kbd>       exit [closewindow] [force]</kbd></li><pre>
   Exit the program, ask for confirm if current file modified.
   if 'closewindow' is given close the window, otherwise leave with a blank schematic
   when closing the last remaining window
   if 'force' is given do not ask before closing modified schematic windows/tabs
   This command returns the list of remaining open windows in addition to main window </pre>
   <li><kbd>       expandlabel lab</kbd></li><pre>
   Expand vectored labels/instance names:
   xschem expandlabel {2*A[3:0]} --&gt; A[3],A[2],A[1],A[0],A[3],A[2],A[1],A[0] 8
   last field is the number of bits
   since [ and ] are TCL special characters argument must be quoted with { and } </pre>
   <li><kbd>       fill_reset [nodraw]</kbd></li><pre>
   After setting tcl array pixdata(n) reset fill patterns on all layers
   If 'nodraw' is given do not redraw window.</pre>
   <li><kbd>       fill_type n fill_type [nodraw]</kbd></li><pre>
   Set fill type for layer 'n', fill_type may be 'solid' or 'stipple' or 'empty'
   If 'nodraw' is given do not redraw window.</pre>
   <li><kbd>       find_nth string sep quote keep_quote n</kbd></li><pre>
   Find n-th field string separated by characters in sep. 1st field is in position 1
   do not split quoted fields (if quote characters are given) and return unquoted.
   xschem find_nth {aaa,bbb,ccc,ddd} {,} 2  --&gt; bbb 
   xschem find_nth {aaa, "bbb, ccc" , ddd} { ,} {"} 2  --&gt; bbb, ccc</pre>
   <li><kbd>       flip [x0 y0]</kbd></li><pre>
   Flip selection horizontally around point x0 y0. 
   if x0, y0 not given use mouse coordinates </pre>
   <li><kbd>       flip_in_place</kbd></li><pre>
   Flip selection horizontally, each object around its center </pre>
   <li><kbd>       flipv [x0 y0]</kbd></li><pre>
   Flip selection vertically around point x0 y0. 
   if x0, y0 not given use mouse coordinates </pre>
   <li><kbd>       flipv_in_place</kbd></li><pre>
   Flip selection vertically, each object around its center </pre>
   <li><kbd>       floaters_from_selected_inst</kbd></li><pre>
   flatten to current level selected instance texts </pre>
   <li><kbd>       fullscreen</kbd></li><pre>
   Toggle fullscreen modes: fullscreen with menu &amp; status, fullscreen, normal </pre>
   <li><kbd>       get var</kbd></li><pre>
   Get C variable/constant 'var' </pre>
   <ul>
     <li><kbd> backlayer </kbd> number of background layer </li>
     <li><kbd> bbox_hilighted </kbd> bounding box of highlinhted objects </li>
     <li><kbd> bbox_selected </kbd> bounding box of selected objects </li>
     <li><kbd> cadlayers </kbd> number of layers </li>
     <li><kbd> case_insensitive </kbd> case_insensitive symbol matching </li>
     <li><kbd> color_ps </kbd> color postscript flag </li>
     <li><kbd> current_dirname </kbd> directory name of current design </li>
     <li><kbd> current_name </kbd> name of current design (no library path) </li>
     <li><kbd> current_win_path </kbd> path of current tab/window (.drw, .x1.drw, ...) </li>
     <li><kbd> currsch </kbd> hierarchy level of current schematic (start at 0) </li>
     <li><kbd> debug_var </kbd> debug level (0 = no debug, 1, 2, 3,...) </li>
     <li><kbd> draw_window </kbd> direct draw into window </li>
     <li><kbd> first_sel </kbd> get data about first selected object </li>
     <li><kbd> fix_broken_tiled_fill </kbd> get drawing method setting (for broken GPUs) </li>
     <li><kbd> fix_mouse_coord </kbd> get fix_mouse_coord setting (fix for broken RDP)</li>
     <li><kbd> format </kbd> alternate format attribute to use in netlist (or NULL) </li>
     <li><kbd> graph_lastsel </kbd> number of last graph that was clicked </li>
     <li><kbd> gridlayer </kbd> layer number for grid </li>
     <li><kbd> help </kbd> command help </li>
     <li><kbd> header_text </kbd> header metadata (license info etc) present in schematic </li>
     <li><kbd> infowindow_text </kbd> ERC messages </li>
     <li><kbd> instances </kbd> number of instances in schematic </li>
     <li><kbd> last_created_window </kbd> return win_path of last created tab or window </li>
     <li><kbd> lastsel </kbd> number of selected objects </li>
     <li><kbd> line_width </kbd> get line width </li>
     <li><kbd> lines </kbd> (xschem get lines n) number of lines on layer 'n' </li>
     <li><kbd> netlist_name </kbd> netlist name if set. If 'fallback' given get default name </li>
     <li><kbd> netlist_type </kbd> get current netlist type (spice/vhdl/verilog/tedax) </li>
     <li><kbd> no_draw </kbd> disable drawing </li>
     <li><kbd> ntabs </kbd> get number of additional tabs (0 = only one tab) </li>
     <li><kbd> pinlayer </kbd> layer number for pins </li>
     <li><kbd> raw_level </kbd> hierarchy level where raw file was loaded </li>
     <li><kbd> rectcolor </kbd> current layer number </li>
     <li><kbd> rects </kbd> (xschem get rects n) number of rectangles on layer 'n' </li>
     <li><kbd> sellayer </kbd> layer number for selection </li>
     <li><kbd> semaphore </kbd> used for debug </li>
     <li><kbd> schname </kbd> get full path of current sch. if 'n' given get sch of level 'n' </li>
     <li><kbd> schprop </kbd> get schematic "spice" global attributes </li>
     <li><kbd> schvhdlprop </kbd> get schematic "vhdl" global attributes </li>
     <li><kbd> schverilogprop </kbd> get schematic "verilog" global attributes </li>
     <li><kbd> schsymbolprop </kbd> get schematic "symbol" global attributes </li>
     <li><kbd> schtedaxprop </kbd> get schematic "tedax" global attributes </li>
     <li><kbd> sch_path </kbd> get hierarchy path. if 'n' given get hierpath of level 'n' </li>
     <li><kbd> sch_to_compare </kbd> if set return schematic current design is compared with </li>
     <li><kbd> temp_dir </kbd> get windows temporary dir </li>
     <li><kbd> text_svg </kbd> return 1 if using &lt;text&gt; elements in svg export </li>
     <li><kbd> textlayer </kbd> layer number for texts </li>
     <li><kbd> top_path </kbd> get top hier path of current window (always "" for tabbed if) </li>
     <li><kbd> topwindow </kbd> same as top_path but main window returned as "." </li>
     <li><kbd> version </kbd> return xschem version </li>
     <li><kbd> wirelayer </kbd> layer used for wires </li>
     <li><kbd> wires </kbd> number of wires </li>
     <li><kbd> xorigin </kbd> x coordinate of origin </li>
     <li><kbd> yorigin </kbd> y coordinate of origin </li>
     <li><kbd> zoom </kbd> zoom level </li>
   </ul>
   <li><kbd>       get_cell cell n_dirs</kbd></li><pre>
   return result of get_cell function </pre>
   <li><kbd>       get_cell_w_ext cell n_dirs</kbd></li><pre>
   return result of get_cell_w_ext function </pre>
   <li><kbd>       getprop instance|instance_pin|symbol|text ref </kbd></li><pre>
      
       getprop instance inst
   Get the full attribute string of 'inst'
      
       getprop instance inst attr
   Get the value of attribute 'attr'
   If 'attr has the form 'cell::sym_attr' look up attribute 'sym_attr'
   of the symbol referenced by the instance.
      
       getprop instance_notcl inst attr
   Same as above but do not perform tcl substitution
      
       getprop instance_pin inst pin
   Get the full attribute string of pin 'pin' of instance 'inst'
   Example: xschem getprop instance_pin x3 MINUS --&gt; name=MINUS dir=in
      
       getprop instance_pin inst pin pin_attr
   Get attribute 'pin_attr' of pin 'pin' of instance 'inst'
   Example: xschem getprop instance_pin x3 MINUS dir --&gt; in
      
       getprop symbol sym_name
   Get full attribute string of symbol 'sym_name'
   example:
   xschem getprop symbol comp_ngspice.sym --&gt;
     type=subcircuit
     format="@name @pinlist @symname
        OFFSET=@OFFSET AMPLITUDE=@AMPLITUDE GAIN=@GAIN ROUT=@ROUT COUT=@COUT"
     template="name=x1 OFFSET=0 AMPLITUDE=5 GAIN=100 ROUT=1000 COUT=1p"
      
       getprop symbol sym_name sym_attr [with_quotes]
   Get value of attribute 'sym_attr' of symbol 'sym_name'
   'with_quotes' (default:0) is an integer passed to get_tok_value()
      
       getprop rect layer num attr [with_quotes]
   if '1' is given as 'keep' return backslashes and unescaped quotes if present in value
   Get attribute 'attr' of rectangle number 'num' on layer 'layer'
      
       getprop text num attr
   Get attribute 'attr' of text number 'num'
   if attribute is 'txt_ptr' return the text
      
       getprop wire num attr
   Get attribute 'attr' of wire number 'num'
    
       ('inst' can be an instance name or instance number)
       ('pin' can be a pin name or pin number)</pre>
   <li><kbd>       get_sch_from_sym inst</kbd></li><pre>
   get schematic associated with instance 'inst' </pre>
   <li><kbd>       get_tok str tok [with_quotes]</kbd></li><pre>
   get value of token 'tok' in string 'str'
   'with_quotes' (default:0) is an integer passed to get_tok_value() </pre>
   <li><kbd>       get_tok_size</kbd></li><pre>
   Get length of last looked up attribute name (not its value) 
   if returned value is 0 it means that last searched attribute did not exist </pre>
   <li><kbd>       globals</kbd></li><pre>
   Return various global variables used in the program </pre>
   <li><kbd>       go_back</kbd></li><pre>
   Go up one level (pop) in hierarchy </pre>
   <li><kbd>       hash_file file [skip_path_lines]</kbd></li><pre>
   Do a simple hash of 'file'
   'skip_path_lines' is an integer (default: 0) passed to hash_file() </pre>
   <li><kbd>       hash_string str</kbd></li><pre>
   Do a simple hashing of string 'str' </pre>
   <li><kbd>       help</kbd></li><pre>
  Print command help </pre>
   <li><kbd>       hier_psprint [file]</kbd></li><pre>
   Hierarchical postscript / pdf print
   if 'file' is not given show a fileselector dialog box </pre>
   <li><kbd>       hilight [drill]</kbd></li><pre>
   Highlight selected element/pins/labels/nets
   if 'drill' is given propagate net highlights through conducting elements
   (elements that have the 'propag' attribute on pins ) </pre>
   <li><kbd>       hilight_instname inst [fast]</kbd></li><pre>
   Highlight instance 'inst' 
       if 'fast' is specified do not redraw 
   'inst' can be an instance name or number </pre>
   <li><kbd>       hilight_netname net</kbd></li><pre>
   Highlight net name 'net' </pre>
   <li><kbd>       instance sym_name x y rot flip [prop] [n]</kbd></li><pre>
   Place a new instance of symbol 'sym_name' at position x,y,
   rotation and flip  set to 'rot', 'flip'
   if 'prop' is given it is the new instance attribute
   string (default: symbol template string)
   if 'n' is given it must be 0 on first call
   and non zero on following calls
   It is used only for efficiency reasons if placing multiple instances </pre>
   <li><kbd>       instance_bbox inst</kbd></li><pre>
   return instance and symbol bounding boxes
   'inst' can be an instance name or number </pre>
   <li><kbd>       instance_coord [instance]</kbd></li><pre>
   Return instance name, symbol name, x placement coord, y placement coord, rotation and flip
   of selected instances 
   if 'instance' is given (instance name or number) return data about specified instance 
   Example:
     xschem [~] xschem instance_coord   
     {R5} {res.sym} 260 260 0 0
     {C1} {capa.sym} 150 150 1 1 </pre>
   <li><kbd>       instance_list</kbd></li><pre>
   Return a list of 3-items. Each 3-item is 
   an instance name followed by the symbol reference and symbol type.
   Example: xschem instance_list --&gt;
     {x1} {sky130_tests/bandgap.sym} {subcircuit}} {...} {...} {...} ... </pre>
   <li><kbd>       instance_net inst pin</kbd></li><pre>
   Return the name of the net attached to pin 'pin' of instance 'inst'
   Example: xschem instance_net x3 MINUS --&gt; REF </pre>
   <li><kbd>       instance_nodemap inst [pin]</kbd></li><pre>
   Return the instance name followed by a list of 'pin net' associations
   example:  xschem instance_nodemap x3
   --&gt; x3 PLUS LED OUT LEVEL MINUS REF
   instance x3 pin PLUS is attached to net LED, pin OUT to net LEVEL and so on...
   If 'pin' is given restrict map to only that pin </pre>
   <li><kbd>       instance_number inst [n]</kbd></li><pre>
   Return the position of instance 'inst' in the instance array 
   If 'n' is given set indicated instance position to 'n' </pre>
   <li><kbd>       instance_pin_coord inst attr value</kbd></li><pre>
   Return the name and coordinates of pin with 
   attribute 'attr' set to 'value' of instance 'inst'
   'inst can be an instance name or a number
   Example: xschem instance_pin_coord x3 name MINUS --&gt; {MINUS} 600 -840 </pre>
   <li><kbd>       instance_pins inst</kbd></li><pre>
   Return list of pins of instance 'inst'
   'inst can be an instance name or a number </pre>
   <li><kbd>       instance_pos inst</kbd></li><pre>
   Get number (position) of instance name 'inst' </pre>
   <li><kbd>       instances_to_net net</kbd></li><pre>
   Return list of instances names and pins attached to net 'net' 
   Example: xschem instances_to_net PANEL
    --&gt; { {Vsw} {plus} {580} {-560} } { {p2} {p} {660} {-440} }
        { {Vpanel1} {minus} {600} {-440} } </pre>
   <li><kbd>       is_symgen symbol</kbd></li><pre>
   tell if 'symbol' is agenerator (symbol(param1,param2,...) </pre>
   <li><kbd>       line [x1 y1 x2 y2] [pos] [propstring] [draw]</kbd></li><pre>
   if 'x1 y1 x2 y2'is given place line on current
   layer (rectcolor) at indicated coordinates.
   if 'pos' is given insert at given position in rectangle array.
   if 'pos' set to -1 append to last element in line array.
   'propstring' is the attribute string. Set to empty if not given.
   if 'draw' is set to 1 (default) draw the new object, else don't
   If no coordinates are given start a GUI operation of line placement </pre>
   <li><kbd>       line_width n</kbd></li><pre>
   set line width to floating point number 'n' </pre>
   <li><kbd>       list_hierarchy</kbd></li><pre>
   List all schematics at or below current hierarchy with modification times.
   Example: xschem list_hiearchy
   --&gt;
   20230302_003134  {/home/.../ngspice/solar_panel.sch}
   20230211_010031  {/home/.../ngspice/pv_ngspice.sch}
   20221011_175308  {/home/.../ngspice/diode_ngspice.sch}
   20221014_091945  {/home/.../ngspice/comp_ngspice.sch}</pre>
   <li><kbd>       list_hilights [sep]</kbd></li><pre>
    Sorted list of highlight nets, separated by character 'sep' (default: space) </pre>
   <li><kbd>       list_tokens str with_quotes</kbd></li><pre>
   List tokens in string 'str'
   with_quotes:
   0: eat non escaped quotes (")
   1: return unescaped quotes as part of the token value if they are present
   2: eat backslashes </pre>
   <li><kbd>       load f [symbol|gui|noundoreset|nofullzoom]</kbd></li><pre>
   Load a new file 'f'.
   'gui': ask to save modified file or warn if opening an already
   open file or opening a new(not existing) file.
   'noundoreset': do not reset the undo history
   'symbol': do not load symbols (used if loading a symbol instead of a schematic)
   'nofullzoom': do not do a full zoom on new schematic.</pre>
   <li><kbd>       load_new_window [f]</kbd></li><pre>
   Load schematic in a new tab/window. If 'f' not given prompt user 
   if 'f' is given as empty '{}' then open untitled.sch </pre>
   <li><kbd>       log f</kbd></li><pre>
   If 'f' is given output stderr messages to file 'f'
   if 'f' is not given and a file log is open, close log
   file and resume logging to stderr </pre>
   <li><kbd>       logic_get_net net_name</kbd></li><pre>
   Get logic state of net named 'net_name'
   Returns 0, 1, 2, 3 for logic levels 0, 1, X, Z or nothing if no net found.</pre>
   <li><kbd>       logic_set_net net_name n [num]</kbd></li><pre>
   set 'net_name' to logic level 'n' 'num' times.
   'n': 
       0  set to logic value 0
       1  set to logic value 1
       2  set to logic value X
       3  set to logic value Z
      -1  toggle logic valie (1-&gt;0, 0-&gt;1)
   the 'num' parameter is essentially useful only with 'toggle' (-1)  value</pre>
   <li><kbd>       logic_set n [num]</kbd></li><pre>
   set selected nets, net labels or pins to logic level 'n' 'num' times.
   'n': 
       0  set to logic value 0
       1  set to logic value 1
       2  set to logic value X
       3  set to logic value Z
      -1  toggle logic valie (1-&gt;0, 0-&gt;1)
   the 'num' parameter is essentially useful only with 'toggle' (-1)  value</pre>
   <li><kbd>       make_sch</kbd></li><pre>
   Make a schematic from selected symbol </pre>
   <li><kbd>       make_sch_from_sel </kbd></li><pre>
   Create an LCC instance from selection and place it instead of selection
   also ask if a symbol (.sym) file needs to be created </pre>
   <li><kbd>       make_symbol</kbd></li><pre>
   From current schematic (circuit.sch) create a symbol (circuit.sym) 
   using ipin.sym, opin.sym, iopin.sym in schematic
   to deduce symbol interface pins. </pre>
   <li><kbd>       merge [f]</kbd></li><pre>
   Merge another file. if 'f' not given prompt user. </pre>
   <li><kbd>       move_instance inst x y rot flip [nodraw] [noundo]</kbd></li><pre>
   resets instance coordinates, and rotaton/flip. A dash will keep existing value
   if 'nodraw' is given do not draw the moved instance
   if 'noundo' is given operation is not undoable </pre>
   <li><kbd>       move_objects [dx dy] [kissing] [stretch]</kbd></li><pre>
   Start a move operation on selection and let user terminate the operation in the GUI
   if kissing is given add nets to pins that touch other instances or nets
   if stretch is given stretch connected nets to follow instace pins 
   if dx and dy are given move by that amount. </pre>
   <li><kbd>       my_strtok_r str delim quote keep_quote</kbd></li><pre>
       test for my_strtok_r() function </pre>
   <li><kbd>       net_label [type]</kbd></li><pre>
   Place a new net label
   'type': 1: place a 'lab_pin.sym' label
           0: place a 'lab_wire.sym' label
   User should complete the placement in the GUI. </pre>
   <li><kbd>       net_pin_mismatch</kbd></li><pre>
   Highlight nets attached to selected symbols with
   a different name than symbol pin </pre>
   <li><kbd>       netlist [-messages] [filename]</kbd></li><pre>
   do a netlist of current schematic in currently defined netlist format 
   if 'filename'is given use specified name for the netlist
   if 'filename' contains path components place the file in specified path location.
   if only a name is given and no path ('/') components are given use the
   default netlisting directory.
   This means that 'xschem netlist test.spice' and 'xschem netlist ./test.spice'
   will create the netlist in different places.
   netlisting directory is reset to previous setting after completing this command
   If -messages is given return the ERC messages instead of just a fail (1) 
   or no fail (0) code. </pre>
   <li><kbd>       new_process [f]</kbd></li><pre>
   Start a new xschem process for a schematic.
   If 'f' is given load specified schematic. </pre>
   <li><kbd>       new_schematic create|destroy|destroy_all|switch winpath file [draw]</kbd></li><pre>
   Open/destroy a new tab or window 
     create: create new empty window or with 'file' loaded if 'file' given.
             The winpath must be given (even {} is ok).
             non empty winpath ({1}) will avoid warnings if opening the
             same file multiple times.
     destroy: destroy tab/window identified by winpath. Example:
              xschem new_schematic destroy .x1.drw
     destroy_all: close all tabs/additional windows
              if the 'force'argument is given do not issue a warning if modified
              tabs are about to be closed.
     switch: switch context to specified 'winpath' window or specified schematic name
              If 'draw' is given and set to 0 do not redraw after switching tab
              (only tab i/f)
   Main window/tab has winpath set to .drw,
   Additional windows/tabs have winpath set to .x1.drw, .x2.drw and so on...</pre>
   <li><kbd>       only_probes</kbd></li><pre>
       dim schematic to better show highlights </pre>
   <li><kbd>       origin x y [zoom]</kbd></li><pre>
   Move origin to 'x, y', optionally changing zoom level to 'zoom'
   A dash ('-') given for x or y will keep existing value </pre>
   <li><kbd>       parse_cmd</kbd></li><pre>
   debug command to test parse_cmd_string()
   splits a command string into argv-like arguments
   return # of args in *argc
   argv[*argc] is always set to NULL </pre>
   <li><kbd>       parselabel str</kbd></li><pre>
   Debug command to test vector net syntax parser </pre>
   <li><kbd>       paste [x y]</kbd></li><pre>
   Paste clipboard. If 'x y' not given user should complete placement in the GUI </pre>
   <li><kbd>       pinlist inst [attr]</kbd></li><pre>
   List all pins of instance 'inst' 
   if no 'attr' is given return full attribute string,
   else return value for attribute 'attr'.
   Example: xschem pinlist x3 name
   --&gt;  { {0} {PLUS} } { {1} {OUT} } { {2} {MINUS} }
   Example: xschem pinlist x3 dir
   --&gt;  { {0} {in} } { {1} {out} } { {2} {in} }
   Example: xschem pinlist x3
   --&gt; { {0} {name=PLUS dir=in } } { {1} {name=OUT dir=out } }
       { {2} {name=MINUS dir=in } }</pre>
   <li><kbd>       place_symbol [sym_name] [prop]</kbd></li><pre>
   Start a GUI placement operation of specified 'sym_name' symbol.
   If 'sym_name' not given prompt user
   'prop' is the attribute string of the symbol.
   If not given take from symbol template attribute.</pre>
   <li><kbd>       place_text </kbd></li><pre>
   Start a GUI placement of a text object </pre>
   <li><kbd>       polygon</kbd></li><pre>
   Start a GUI placement of a polygon </pre>
   <li><kbd>       preview_window create|draw|destroy [winpath] [file]</kbd></li><pre>
   Used in fileselector to show a schematic preview.</pre>
   <li><kbd>       print png|svg|ps|pdf|ps_full|pdf_full img_file [img_x img_y] [x1 y1 x2 y2]</kbd></li><pre>
   If img_x and img_y are set to 0 (recommended for svg and ps/pdf) 
   they will be calculated by xschem automatically
   Export current schematic to image.
                            img x   y size    xschem area to export
      0     1    2    3         4   5             6    7   8   9
   xschem print png file.png  [400 300]       [ -300 -200 300 200 ]
   xschem print svg file.svg  [400 300]       [ -300 -200 300 200 ]
   xschem print ps  file.ps   [400 300]       [ -300 -200 300 200 ]
   xschem print eps file.eps  [400 300]       [ -300 -200 300 200 ]
   xschem print pdf file.pdf  [400 300]       [ -300 -200 300 200 ]
   xschem print ps_full  file.ps
   xschem print pdf_full file.pdf</pre>
   <li><kbd>       print_hilight_net show</kbd></li><pre>
   from highlighted nets/pins/labels:
   show == 0   ==&gt; create pins from highlight nets
   show == 1   ==&gt; show list of highlight net in a dialog box
   show == 2   ==&gt; create labels with i prefix from hilight nets
   show == 3   ==&gt; show list of highlight net with path and label
                  expansion in a dialog box
   show == 4   ==&gt; create labels without i prefix from hilight nets
   for show = 0, 2, 4 user should complete GUI placement
   of created objects </pre>
   <li><kbd>       print_spice_element inst</kbd></li><pre>
   Print spice raw netlist line for instance (number or name) 'inst' </pre>
   <li><kbd>       propagate_hilights [set clear] </kbd></li><pre>
   Debug: wrapper to propagate_hilights() function </pre>
   <li><kbd>       push_undo</kbd></li><pre>
   Push current state on undo stack </pre>
   <li><kbd>       raw what [rawfile type] [sweep1 sweep2]</kbd></li><pre>
       what = read | clear | info | switch | switch_back
   Load / clear / switch additional raw files
   if sweep1, sweep2 interval is given in 'read' subcommand load only the interval
   sweep1 &lt;= sweep_var &lt; sweep2 </pre>
   <li><kbd>       raw_clear </kbd></li><pre>
   Unload all simulation raw files </pre>
   <li><kbd>       raw_query loaded|value|index|values|datasets|vars|list </kbd></li><pre>
   xschem raw_query list: get list of saved simulation variables
   xschem raw_query vars: get number of simulation variables
   xschem raw_query datasets: get number of datasets (simulation runs)
   xschem raw_query value node n [dataset]: return n-th value of 'node' in raw file
     If n is egiven as empty string {} return value at cursor b, dataset not used in this case
   xschem raw_query loaded: return hierarchy level
   where raw file was loaded or -1 if no raw loaded
   xschem raw_query rawfile: return raw filename 
   xschem raw_query sim_type: return raw loaded simulation type (ac, op, tran, ...) 
   xschem raw_query index node: get index of simulation variable 'node'. 
     Example:  raw_query index v(led) --&gt; 46
   xschem raw_query values node [dset] : print all simulation
   values of 'node' for dataset 'dset' (default dset=0)
   xschem raw_query points [dset] : print simulation points for
   dataset 'dset' (default: all dataset points combined)</pre>
   <li><kbd>       raw_read [file] [sim] [sweep1 sweep2]</kbd></li><pre>
   If a raw file is already loaded delete from memory
   then load specified file and analysis 'sim' (dc, ac, tran, op, ...)
   If 'sim' not specified load first section found in raw file.
   if sweep1, sweep2 interval is given load only the interval
   sweep1 &lt;= sweep_var &lt; sweep2 </pre>
   <li><kbd>       raw_read_from_attr [sim]</kbd></li><pre>
   If a simulation raw file is already loaded delete from memory
   else read section 'sim' (tran, dc, ac, op, ...)
   of base64 encoded data from a 'spice_data'
   attribute of selected instance
   If sim not given read first section found </pre>
   <li><kbd>       rebuild_connectivity </kbd></li><pre>
   Rebuild logical connectivity abstraction of schematic </pre>
   <li><kbd>       rebuild_selection </kbd></li><pre>
   Rebuild selection list</pre>
   <li><kbd>       record_global_node n node </kbd></li><pre>
   call the record_global_node function (list of netlist global nodes) </pre>
   <li><kbd>       rect [x1 y1 x2 y2] [pos] [propstring] [draw]</kbd></li><pre>
   if 'x1 y1 x2 y2'is given place recangle on current
   layer (rectcolor) at indicated coordinates.
   if 'pos' is given insert at given position in rectangle array.
   if 'pos' set to -1 append rectangle to last element in rectangle array.
   'propstring' is the attribute string. Set to empty if not given.
   if 'draw' is set to 1 (default) draw the new object, else don't
   If no coordinates are given start a GUI operation of rectangle placement </pre>
   <li><kbd>       redo</kbd></li><pre>
   Redo last undone action </pre>
   <li><kbd>       redraw</kbd></li><pre>
   redraw window </pre>
   <li><kbd>       reload</kbd></li><pre>
   Forced (be careful!) Reload current schematic from disk </pre>
   <li><kbd>       reload_symbols</kbd></li><pre>
   Reload all used symbols from disk </pre>
   <li><kbd>       remove_symbols</kbd></li><pre>
   Internal command: remove all symbol definitions </pre>
   <li><kbd>       replace_symbol inst new_symbol [fast]</kbd></li><pre>
   Replace 'inst' symbol with 'new_symbol'
   If doing multiple substitutions set 'fast' to {}
    on first call and 'fast' on next calls
   for faster operation.
   do a 'xschem redraw' at end to update screen
   Example: xschem replace_symbol R3 capa.sym </pre>
   <li><kbd>       reset_caches</kbd></li><pre>
   Reset cached instance and symbol cached flags (inst-&gt;flags, sym-&gt;flags) </pre>
   <li><kbd>       reset_symbol inst symref</kbd></li><pre>
   This is a low level command, it merely changes the xctx-&gt;inst[...].name field.
   It is caller responsibility to delete all symbols before and do a reload_symbols
   afterward </pre>
   <li><kbd>       resetwin create_pixmap clear_pixmap force w h</kbd></li><pre>
   internal command: calls resetwin() </pre>
   <li><kbd>       resolved_net [net]</kbd></li><pre>
   if 'net' is given  return its topmost full hierarchy name
   else returns the topmost full hierarchy name of selected net/pin/label.
   Nets connected to I/O ports are mapped to upper level recursively </pre>
   <li><kbd>       rotate [x0 y0]</kbd></li><pre>
   Rotate selection around point x0 y0. 
   if x0, y0 not given use mouse coordinates </pre>
   <li><kbd>       rotate_in_place</kbd></li><pre>
   Rotate selected objects around their 0,0 coordinate point </pre>
   <li><kbd>       save</kbd></li><pre>
   Save schematic if modified. Does not ask confirmation! </pre>
   <li><kbd>       saveas [file] [type]</kbd></li><pre>
   save current schematic as 'file'
   if file is empty ({}) use current schematic name
   as defalt and prompt user with file selector
   'type' is used used to set/change file extension:
     schematic: save as schematic (*.sch)
     symbol: save as symbol (*.sym)
     If not specified default to schematic (*.sch)
   Does not ask confirmation if file name given</pre>
   <li><kbd>       sch_pinlist</kbd></li><pre>
   List a 2-item list of all pins  and directions of current schematic
   Example: xschem sch_pinlist
   --&gt;  {PLUS} {in} {OUT} {out} {MINUS} {in} {VCC} {inout} {VSS} {inout}</pre>
   <li><kbd>       schematic_in_new_window [new_process] [nodraw] [force]</kbd></li><pre>
   When a symbol is selected edit corresponding schematic
   in a new tab/window if not already open.
   If nothing selected open another window of the second
   schematic (issues a warning).
   if 'new_process' is given start a new xschem process
   if 'nodraw' is given do not draw loaded schematic
   returns '1' if a new schematic was opened, 0 otherwise </pre>
   <li><kbd>       search regex|exact select tok val [match_case]</kbd></li><pre>
   Search instances / wires / rects / texts with attribute string containing 'tok'
   and value 'val'
   search can be exact ('exact') or as a regular expression ('regex')
   select: 
      0 : highlight matching instances
      1 : select matching instances
     -1 : unselect matching instances 
   'tok' set as:
       propstring : will search for 'val' in the entire 
       *instance* attribute string.
       cell::propstring : will search for 'val' in the entire
       *symbol* attribute string. 
       cell::name : will search for 'val' in the symbol name
       cell::&lt;attr&gt; will search for 'val' in symbol attribute 'attr'
         example: xschem search regex 0 cell::template GAIN=100
    match_case:
      1 : Match case
      0 : Do not match case
      If not given assume 1 (Match case)</pre>
   <li><kbd>       select instance|wire|text id [clear] [fast]</kbd></li><pre>
       select rect|line|poly|arc layer id [clear] [fast]
       Select indicated instance or wire or text, or
       Select indicated (layer, number) rectangle, line, polygon, arc.
       For 'instance' 'id' can be the instance name or number
       for all other objects 'id' is the position in the respective arrays
       if 'clear' is specified does an unselect operation
       if 'fast' is specified avoid sending information to infowindow and status bar
       returns 1 if something selected, 0 otherwise </pre>
   <li><kbd>       select_all</kbd></li><pre>
   Selects all objects in schematic </pre>
   <li><kbd>       select_dangling_nets </kbd></li><pre>
   Select all nets/labels that are dangling, ie not attached to any non pin/port/probe components
   Returns number of selected items (wires,labels) if danglings found, 0 otherwise </pre>
   <li><kbd>       select_hilight_net</kbd></li><pre>
   Select all highlight objects (wires, labels, pins, instances) </pre>
   <li><kbd>       select_inside x1 y1 x2 y2 [sel]</kbd></li><pre>
   Select all objects inside the indicated area
   if [sel] is set to '0' do an unselect operation </pre>
   <li><kbd>       selected_set [what]</kbd></li><pre>
   Return a list of selected instance names
   If what is not given or set to 'inst' return list of selected instance names
   If what set to 'rect' return list of selected rectangles with their coordinates
   If what set to 'text' return list of selected texts with their coordinates </pre>
   <li><kbd>       selected_wire</kbd></li><pre>
  Return list of selected nets </pre>
   <li><kbd>       send_to_viewer</kbd></li><pre>
   Send selected wires/net labels/pins/voltage source or ammeter currents to current
   open viewer (gaw or bespice) </pre>
   <li><kbd>       set var value</kbd></li><pre>
   Set C variable 'var' to 'value' </pre>
   <ul>
     <li><kbd> cadgrid </kbd> set cad grid (default: 20) </li>
     <li><kbd> cadsnap </kbd> set mouse snap (default: 10) </li>
     <li><kbd> color_ps </kbd> set color psoscript (1 or 0) </li>
     <li><kbd> constrained_move </kbd> set constrained move (1=horiz, 2=vert, 0=none) </li>
     <li><kbd> cursor1_x </kbd> set graph cursor1 position </li>
     <li><kbd> cursor2_x </kbd> set graph cursor2 position </li>
     <li><kbd> draw_window </kbd> set drawing to window (1 or 0) </li>
     <li><kbd> fix_broken_tiled_fill </kbd> alternate drawing method for broken GPUs </li>
     <li><kbd> fix_mouse_coord </kbd> fix for wrong mouse coords in RDP software </li>
     <li><kbd> format </kbd> set name of custom format attribute used for netlisting </li>
     <li><kbd> header_text </kbd> set header metadata (used for license info) </li>
     <li><kbd> hide_symbols </kbd> set to 0,1,2 for various hiding level of symbols </li>
     <li><kbd> hilight_color </kbd> set hilight color for next hilight </li>
     <li><kbd> infowindow_text </kbd> ERC messages </li>
     <li><kbd> netlist_name </kbd> set custom netlist name </li>
     <li><kbd> netlist_type </kbd> set netlisting mode (spice, verilog, vhdl, tedax, symbol) </li>
     <li><kbd> no_draw </kbd> set no drawing flag (0 or 1) </li>
     <li><kbd> no_undo </kbd> set to 1 to disable undo </li>
     <li><kbd> raw_level </kbd> set hierarchy level loaded raw file refers to </li>
     <li><kbd> rectcolor </kbd> set current layer (0, 1, .... , cadlayers-1) </li>
     <li><kbd> sch_to_compare </kbd> set name of schematic to compare current window with </li>
     <li><kbd> schsymbolprop </kbd> set global symbol attribute string </li>
     <li><kbd> schprop </kbd> set schematic global spice attribute string </li>
     <li><kbd> schverilogprop </kbd> set schematic global verilog attribute string </li>
     <li><kbd> schvhdlprop </kbd> set schematic global vhdl attribute string </li>
     <li><kbd> schtedaxprop </kbd> set schematic global tedax attribute string </li>
     <li><kbd> text_svg </kbd> set to 1 to use svg &lt;text&gt; elements </li>
     <li><kbd> semaphore </kbd> debug </li>
     <li><kbd> show_hidden_texts </kbd> set to 1 to enable showing texts with attr hide=true </li>
     <li><kbd> sym_txt </kbd> set to 0 to hide symbol texts </li>
   </ul>
   <li><kbd>       set_different_tok str new_str old_str</kbd></li><pre>
   Return string 'str' replacing/adding/removing tokens that are
   different between 'new_str' and 'old_str' </pre>
   <li><kbd>       set_modify</kbd></li><pre>
   Force modify status on current schematic </pre>
   <li><kbd>       setprop instance|symbol|text|rect ref tok [val] [fast]</kbd></li><pre>
      
       setprop instance inst tok [val] [fast]
   set attribute 'tok' of instance (name or number) 'inst' to value 'val'
   If 'val' not given (no attribute value) delete attribute from instance
   If 'fast' argument if given does not redraw and is not undoable 
      
       setprop symbol name tok [val]
   Set attribute 'tok' of symbol name 'name' to 'val'
   If 'val' not given (no attribute value) delete attribute from symbol
      
       setprop rect lay n tok [val] [fast|fastundo]
   Set attribute 'tok' of rectangle number'n' on layer 'lay'
   If 'val' not given (no attribute value) delete attribute from rect
   If 'fast' argument is given does not redraw and is not undoable
   If 'fastundo' s given same as above but action is undoable.
      
       setprop rect 2 n fullxzoom
       setprop rect 2 n fullyzoom
   These commands do full x/y zoom of graph 'n' (on layer 2, this is hardcoded).
      
       setprop text n [tok] [val] [fast|fastundo]
   Set attribute 'tok' of text number 'n'
   If 'tok' not specified set text string (txt_ptr) to value
   If "txt_ptr" is given as token replace the text txt_ptr ("the text")
   If 'val' not given (no attribute value) delete attribute from text
   If 'fast' argument is given does not redraw and is not undoable
   If 'fastundo' s given same as above but action is undoable.</pre>
   <li><kbd>       simulate [callback]</kbd></li><pre>
   Run a simulation (start simulator configured as default in
   Tools -&gt; Configure simulators and tools) 
   If 'callback' procedure name is given execute the procedure when simulation
   is finished. all execute(..., id) data is available (id = execute(id) )
   A callback prodedure is useful if simulation is launched in background mode
   ( set sim(spice,1,fg) 0 ) </pre>
   <li><kbd>       snap_wire </kbd></li><pre>
   Start a GUI start snapped wire placement (click to start a
   wire to closest pin/net endpoint) </pre>
   <li><kbd>       str_replace str rep with [escape]</kbd></li><pre>
   replace 'rep' with 'with' in string 'str' 
   if rep not preceeded by an 'escape' character </pre>
   <li><kbd>       subst_tok str tok newval</kbd></li><pre>
   Return string 'str' with 'tok' attribute value replaced with 'newval' </pre>
   <li><kbd>       symbol_in_new_window [new_process]</kbd></li><pre>
   When a symbol is selected edit it in a new tab/window if not already open.
   If nothing selected open another window of the second schematic (issues a warning).
   if 'new_process' is given start a new xschem process </pre>
   <li><kbd>       swap_windows </kbd></li><pre>
   swap first and second window in window interface (internal command)</pre>
   <li><kbd>       switch [window_path |schematic_name]</kbd></li><pre>
   Switch context to indicated window path or schematic name
   returns 0 if switch was successfull or 1 in case of errors
   (no tabs/windows present or no matching winpath / schematic name
   found).</pre>
   <li><kbd>       symbols [n]</kbd></li><pre>
   if 'n' given list symbol with name or number 'n', else 
   list all used symbols </pre>
   <li><kbd>       tab_list</kbd></li><pre>
   list all windows / tabs with window pathname and associated filename </pre>
   <li><kbd>       table_read [table_file]</kbd></li><pre>
   If a simulation raw file is lodaded unload from memory.
   else read a tabular file 'table_file'
   First line is the header line containing variable names.
   data is presented in column format after the header line
   First column is sweep (x-axis) variable
   Double empty lines start a new dataset
   Single empty lines are ignored
   Datasets can have different # of lines.
   new dataset do not start with a header row.
   Lines beginning with '#' are comments and ignored
      
      time    var_a   var_b   var_c
   # this is a comment, ignored
       0.0     0.0     1.8    0.3
     &lt;single empty line: ignored&gt;
       0.1     0.0     1.5    0.6
       ...     ...     ...    ...
     &lt;empty line&gt;
     &lt;Second empty line: start new dataset&gt;
       0.0     0.0     1.8    0.3
       0.1     0.0     1.5    0.6
       ...     ...     ...    ...</pre>
   <li><kbd>       test</kbd></li><pre>
   Testmode ... </pre>
   <li><kbd>       text x y rot flip text props size draw</kbd></li><pre>
   Create a text object
     x, y, rot, flip specify the position and orientation
     text is the text string
     props is the attribute string
     size sets the size
     draw is a flag. If set to 1 will draw the created text </pre>
   <li><kbd>       text_string n</kbd></li><pre>
   get text string of text object 'n' </pre>
   <li><kbd>       toggle_colorscheme</kbd></li><pre>
   Toggle dark/light colorscheme </pre>
   <li><kbd>       toggle_ignore</kbd></li><pre>
   toggle *_ignore=true attribute on selected instances
   * = {spice,verilog,vhdl,tedax} depending on current netlist mode </pre>
   <li><kbd>       touch x1 y1 x2 y2 x0 y0</kbd></li><pre>
   returns 1 if line {x1 y1 x2 y2} touches point {x0 y0}, 0 otherwise </pre>
   <li><kbd>       translate n str</kbd></li><pre>
   Translate string 'str' replacing @xxx tokens with values in instance 'n' attributes
     Example: xschem translate vref {the voltage is @value}
     the voltage is 1.8 </pre>
   <li><kbd>       trim_chars str sep</kbd></li><pre>
   Remove leading and trailing chars matching any character in 'sep' from str </pre>
   <li><kbd>       trim_wires</kbd></li><pre>
   Remove operlapping wires, join lines, trim wires at intersections </pre>
   <li><kbd>       undo</kbd></li><pre>
   Undo last action </pre>
   <li><kbd>       undo_type disk|memory</kbd></li><pre>
   Use disk file ('disk') or RAM ('memory') for undo bufer</pre>
   <li><kbd>       unhilight_all [fast]</kbd></li><pre>
   if 'fast' is given do not redraw
   Clear all highlights </pre>
   <li><kbd>       unhilight</kbd></li><pre>
   Unhighlight selected nets/pins </pre>
   <li><kbd>       unselect_all [draw]</kbd></li><pre>
   Unselect everything. If draw is given and set to '0' no drawing is done </pre>
   <li><kbd>       update_all_sym_bboxes</kbd></li><pre>
   Update all symbol bounding boxes (useful if show_pin_net_names is set) </pre>
   <li><kbd>       update_op</kbd></li><pre>
   update tcl ngspice::ngspice array data from raw file point 0 </pre>
   <li><kbd>       view_prop</kbd></li><pre>
   View attributes of selected element (read only)
   if multiple selection show the first element (in xschem  array order) </pre>
   <li><kbd>       warning_overlapped_symbols [sel]</kbd></li><pre>
   Highlight or select (if 'sel' set to 1) perfectly overlapped instances
   this is usually an error and difficult to grasp visually </pre>
   <li><kbd>       windowid topwin_path</kbd></li><pre>
   Used by xschem.tcl for configure events (set icon) </pre>
   <li><kbd>       wire_coord n</kbd></li><pre>
   return 4 coordinates of wire[n] </pre>
   <li><kbd>       wire [x1 y1 x2 y2] [pos] [prop] [sel]</kbd></li><pre>
   Place a new wire
   if no coordinates are given start a GUI wire placement </pre>
   <li><kbd>       wire_cut [x y] [noalign]</kbd></li><pre>
   start a wire cut operation. Point the mouse in the middle of a wire and
   Alt-click right button.
   if x and y are given cut wire at given point
   if noalign is given and is set to 'noalign' do not align the cut point to closest snap point </pre>
   <li><kbd>       xcb_info</kbd></li><pre>
   For debug </pre>
   <li><kbd>       zoom_box [x1 y1 x2 y2] [factor]</kbd></li><pre>
   Zoom to specified coordinates, if 'factor' is given reduce view (factor &lt; 1.0) 
   or add border (factor &gt; 1.0)
   If no coordinates are given start GUI zoom box operation </pre>
   <li><kbd>       zoom_full [center|nodraw|nolinewidth]</kbd></li><pre>
   Set full view. 
   If 'center' is given center vire instead of lower-left align
   If 'nodraw' is given don't redraw
   If 'nolinewidth]' is given don't reset line widths. </pre>
   <li><kbd>       zoom_hilighted </kbd></li><pre>
   Zoom to highlighted objects </pre>
   <li><kbd>       zoom_in</kbd></li><pre>
   Zoom in drawing </pre>
   <li><kbd>       zoom_out</kbd></li><pre>
   Zoom out drawing </pre>
   <li><kbd>       zoom_selected</kbd></li><pre>
   Zoom to selection </pre>






















































 </ul>

  <!-- TCL global variables -->
 <h1>XSCHEM <a id="tclglobals">TCL GLOBAL</a> VARIABLES</h1><br>

 <pre class="code">
   # default command for first spice simulation command (interactive ngspice) 
   sim(spice,0,cmd) {$terminal -e 'ngspice -i "$N" -a || sh'}

   # flag for foreground (1) or background (0) operation
   sim(spice,0,fg) 0

   # flag for status dialog box opening (1) at simulation end or not (0)
   sim(spice,0,st) 0

   sim(spice,1,cmd) {ngspice -b -r "$n.raw" -o "$n.out" "$N"}
   sim(spice,1,fg) 0
   sim(spice,1,st) 1
   sim(spice,2,cmd) "Xyce \"\$N\"\n# Add -r \"\$n.raw\" if you want all variables saved"
   sim(spice,2,fg) 0
   sim(spice,2,st) 1
   sim(spice,3,cmd) {mpirun /path/to/parallel/Xyce "$N"}
   sim(spice,3,fg) 0
   sim(spice,3,st) 1

   # Number of configured spice simulation commands (4), [ sim(spice,0,...) ... sim(spice,3,...) ]
   sim(spice,n) 4

   # default spice command to use (0) --&gt; sim(spice,0,...)
   sim(spice,default) 0

   sim(spicewave,0,cmd) {gaw "$n.raw" } 
   sim(spicewave,0,fg) 0
   sim(spicewave,0,st) 0
   sim(spicewave,1,cmd) {$terminal -e ngspice}
   sim(spicewave,1,fg) 0
   sim(spicewave,1,st) 0
   sim(spicewave,2,cmd) {rawtovcd -v 1.5 "$n.raw" &gt; "$n.vcd" &amp;&amp; gtkwave "$n.vcd" "$n.sav" 2&gt;/dev/null} 
   sim(spicewave,2,fg) 0
   sim(spicewave,2,st) 0
   sim(spicewave,3,cmd) {$env(HOME)/analog_flavor_eval/bin/bspwave --socket localhost $bespice_listen_port "$n.raw" } 
   sim(spicewave,3,fg) 0
   sim(spicewave,3,st) 0
   sim(spicewave,n) 4
   sim(spicewave,default) 0

   # list of configured tools. For each of these there is a set of sim(tool,...) settings
   sim(tool_list) spice spicewave verilog verilogwave vhdl vhdlwave

   sim(verilog,0,cmd) {iverilog -o .verilog_object -g2012 "$N" &amp;&amp; vvp .verilog_object}
   sim(verilog,0,fg) 0
   sim(verilog,0,st) 1
   sim(verilog,n) 1
   sim(verilog,default) 0
   sim(verilogwave,0,cmd) {gtkwave dumpfile.vcd "$N.sav" 2&gt;/dev/null}
   sim(verilogwave,0,fg) 0
   sim(verilogwave,0,st) 0
   sim(verilogwave,n) 1
   sim(verilogwave,default) 0
   sim(vhdl,0,cmd) {ghdl -c --ieee=synopsys -fexplicit "$N" -r "$s" --wave="$n.ghw"}
   sim(vhdl,0,fg) 0
   sim(vhdl,0,st) 1
   sim(vhdl,n) 1
   sim(vhdl,default) 0
   sim(vhdlwave,0,cmd) {gtkwave "$n.ghw" "$N.sav" 2&gt;/dev/null}
   sim(vhdlwave,0,fg) 0
   sim(vhdlwave,0,st) 0
   sim(vhdlwave,n) 1
   sim(vhdlwave,default) 0

   add_all_windows_drives 1
   autofocus_mainwindow 1
   auto_hilight 0
   autotrim_wires 0
   bespice_listen_port {}
   bespice_server_getdata
   big_grid_points 0
   bus_replacement_char {} ;# use {&lt;&gt;} to replace [] with &lt;&gt; in bussed signals
   cadlayers 22
   cairo_font_line_spacing 1.0
   cairo_font_name {Sans-Serif}
   cairo_font_scale 1.0
   cairo_vert_correct 0
   case_insensitive 0
   change_lw 1
   color_ps 1
   colors $dark_colors
   compare_sch 0
   component_browser_on_top 1
   connect_by_kissing 0
   constrained_move 0
   copy_cell 0
   dark_colors {
     "#000000" "#00ccee" "#3f3f3f" "#cccccc" "#88dd00" "#bb2200" "#00ccee" "#ff0000"
     "#ffff00" "#ffffff" "#ff00ff" "#00ff00" "#0044dd" "#aaaa00" "#aaccaa" "#ff7777"
     "#bfff81" "#00ffcc" "#ce0097" "#d2d46b" "#ef6158" "#fdb200"}
   dark_colorscheme 1
   dark_colors_save
   debug_var 0
   delay_flag
   dim_bg 0.0
   dim_value 0.0
   dircolor(/share/doc/xschem/) {#338844}
   dircolor(/share/xschem/) red
   disable_unique_names 0
   download_url_helper {curl -f -s -O}
   draw_grid 1
   draw_window 0
   editor {gvim -f}
   edit_prop_size 80x12
   edit_symbol_prop_new_sel {}
   enable_dim_bg 0
   enable_layer($i) 1
   enable_stretch 0
   en_hilight_conn_inst 0
   execute(cmd,&lt;id&gt;)
   execute(data,&lt;id&gt;)
   execute(status,&lt;id&gt;)
   execute(cmd,last)
   execute(data,last)
   execute(status,last)
   execute(error,last)
   execute(exitcode,last)
   execute(id)
   flat_netlist 0
   fullscreen 0
   gaw_tcp_address {localhost 2020}
   graph_bus 0
   graph_logx 0
   graph_logy 0
   graph_rainbow 0
   graph_raw_level -1 ;# hierarchy level where raw file has been loaded 
   graph_schname {}
   graph_sel_color 4
   graph_selected {}
   graph_sel_wave {}
   graph_sort 0
   has_cairo 1
   has_x
   hide_empty_graphs 0 ;# if set to 1 waveform boxes will be hidden if no raw file loaded
   hide_symbols 0
   incr_hilight 1

   # text saved into the ERC informational dialog box.
   # netlist warnings and errors are shown here.
   infowindow_text 

   initial_geometry {900x600}
   launcher_default_program {xdg-open}
   light_colors {
     "#ffffff" "#0044ee" "#aaaaaa" "#222222" "#229900" "#bb2200" "#00ccee" "#ff0000"
     "#888800" "#00aaaa" "#880088" "#00ff00" "#0000cc" "#666600" "#557755" "#aa2222"
     "#7ccc40" "#00ffcc" "#ce0097" "#d2d46b" "#ef6158" "#fdb200"}
   light_colors_save
   line_width 0
   live_cursor2_backannotate 0

   # if set use &lt;sch_dir&gt;/simulation for netlist and sims
   local_netlist_dir 0

   lvs_ignore 0
   lvs_netlist 0
   measure_text "y=\nx="
   menu_debug_var 0
   myload_files2 {}
   myload_globfilter {*}
   myload_index1 0
   netlist_dir "$USER_CONF_DIR/simulations"
   netlist_show 0
   netlist_type spice
   nocairo_font_xscale .85
   nocairo_font_yscale .88
   nocairo_vert_correct 0
   no_change_attrs 0
   nolist_libs {}
   noprint_libs {}
   only_probes 0  ; # 20110112
   OS
   persistent_command 0
   preserve_unchanged_attrs 0
   rainbow_colors 0
   search_schematic 0
   show_hidden_texts 0
   show_infowindow 0 
   show_infowindow_after_netlist 0
   show_pin_net_names 0
   spiceprefix 1
   split_files 0
   svg_font_name {Sans-Serif}
   symbol_width 150
   sym_txt 1
   tabbed_interface 0
   tcl_files {}
   tclstop 0
   terminal xterm
   text_line_default_geometry 80x12
   textwindow_wcounter
   toolbar_horiz   1
   toolbar_list {  ... }
   toolbar_visible 0
   to_pdf {ps2pdf}
   to_png {gm convert} 
   transparent_svg 0
   undo_type disk
   unzoom_nodrift 0
   use_tclreadline 1 ;# use the tclreadline package for command prompt. default: 1
   USER_CONF_DIR
   verilog_2001 1
   verilog_bitblast 0
   viewdata_wcounter
   xschem_libs {}
   xschem_listen_port {}
   xschem_server_getdata
   XSCHEM_SHAREDIR
   XSCHEM_START_WINDOW {}
   XSCHEM_TMP_DIR {/tmp}
   zoom_full_center 0
 </pre>

 <h3> Simulator / waveform setup </h3>

 <p>
  In xschem a tcl array variable <kbd>sim</kbd> is used to specify external process commands,
  like simulators and waveform viewers. This variable is set in the GUI with the 
  <kbd>Simulation-&gt; Configure simulators and tools</kbd> menu entry. First of all you need to set the 
  <kbd>tool_list</kbd> list of configured tools:</p>
  <pre class = "code">
     set sim(tool_list) { spice spicewave verilog verilogwave vhdl vhdlwave } </pre>
 <p>
  For each tool you need to define some sub elements:</p>
  <pre class = "code">
     # Number of configured spice simulation commands (4), [ sim(spice,0,...) ... sim(spice,3,...) ]
     sim(spice,n) 4
     # default spice command to use (0) --&gt; sim(spice,0,...)
     sim(spice,default) 0
     # default command for first spice simulation command (interactive ngspice)
     sim(spice,0,cmd) {$terminal -e 'ngspice -i "$N" -a || sh'}
     # flag for foreground (1) or background (0) operation
     sim(spice,0,fg) 0
     # flag for status dialog box opening (1) at simulation end or not (0)
     sim(spice,0,st) 0
     sim(spice,1,cmd) {ngspice -b -r "$n.raw" -o "$n.out" "$N"}
     sim(spice,1,fg) 0
     sim(spice,1,st) 1
     sim(spice,2,cmd) "Xyce \"\$N\"\n# Add -r \"\$n.raw\" if you want all variables saved"
     sim(spice,2,fg) 0
     sim(spice,2,st) 1
     sim(spice,3,cmd) {mpirun /path/to/parallel/Xyce "$N"}
     sim(spice,3,fg) 0
     sim(spice,3,st) 1
  </pre>
 
  <!-- TCL procedures -->
 <h1>XSCHEM <a id="tclprocs">TCL PROCEDURES</a></h1><br>
 <p> Commands in brackets are internal procedures, not supposed to be used by end users </p>
 <pre class = "code">
      # show xschem about dialog
      about

      # given a symbol reference 'sym' return its absolute path
      # Example: % abs_sym_path devices/iopin.sch
      #          /home/schippes/share/xschem/xschem_library/devices/iopin.sym
      abs_sym_path sym

      add_ext
      add_lab_no_prefix
      add_lab_prefix

      # show an alert dialog box and display 'text'.
      # if 'position' is empty (example: alert_ {hello, world} {}) show at mouse coordinates
      # otherwise use specified coordinates example: alert_ {hello, world} +300+400
      # if nowait is 1 do not wait for user to close dialog box
      # if yesnow is 1 show yes and no buttons and return user choice (1 / 0).
      # (this works only if nowait is unset).
      alert_ text [position] [nowait] [yesno]

      ask_save
      attach_labels_to_inst
      balloon
      balloon_show
      bespice_getdata
      bespice_server
      build_widgets
      change_color
      clear_simulate_button
      color_dim
      context_menu
      convert_to_pdf
      convert_to_png
      create_layers_menu
      create_pins

      # pause execution for 'ms milliseconds, keeping event loop responding
      delay [ms]
      delete_ctx
      delete_files
      delete_tab
      descend_hierarchy
      download_url
      edit_file
      edit_netlist
      edit_prop
      edit_vi_netlist_prop
      edit_vi_prop
      enter_text

      # evaluate 'expr'. if 'expr' has errors or does not evaluate return 'expr' as is
      ev expr

      every
      execute
      execute_fileevent
      execute_wait
      fill_graph_listbox

      # find file into $paths directories matching $f
      # use $pathlist global search path if $paths empty
      # recursively descend directories
      find_file f [paths]

      # as above, return only first match found
      find_file_first f [paths]

      # process all symbols in current design, get full path of them if found in 
      # XSCHEM_LIBRARY_PATH search path, then transform them with exactly one 'n_dir'
      # path components added.
      # example: current design has an instance referencing 'lab_pin.sym'
      #          after executing 'fix_symbols 1' the instance symbol reference
      #          will be devices/lab_pin.sym. This will be done only on symbols
      #          that are existing in the current search paths (there is
      #          devices/lab_pin.sym in one of the search paths).
      fix_symbols n_dirs

      from_eng
      gaw_cmd
      gaw_echoline
      get_cell
      get_directory
      get_file_path

      # launch a terminal shell, if 'curpath' is given set path to 'curpath'
      get_shell

      graph_add_nodes
      graph_add_nodes_from_list
      graph_change_wave_color
      graph_edit_properties
      graph_edit_wave
      graph_get_signal_list
      graph_show_measure
      graph_update_nodelist
      hash_string
      history
      housekeeping_ctx
      infowindow
      input_line
      inutile
      inutile_alias_window
      inutile_get_time
      inutile_help_window
      inutile_line
      inutile_read_data
      inutile_template
      inutile_translate
      inutile_write_data
      is_xschem_file
      key_binding
      launcher
      list_hierarchy
      list_tokens
      load_file_dialog
      load_file_dialog_mkdir
      load_file_dialog_up
      load_recent_file
      make_symbol
      make_symbol_lcc

      # find files into $paths directories matching $f
      # use $pathlist global search path if $paths empty
      # recursively descend directories
      match_file f [paths]

      myload_display_preview
      myload_getresult
      myload_place_symbol
      myload_set_colors1
      myload_set_colors2
      myload_set_home
      netlist
      next_tab
      no_open_dialogs
      order
      pack_tabs
      pack_widgets
      path_head
      pin_label
      prev_tab
      print_help_and_exit
      probe_net
      property_search

      # quit xschem closing all tabs/windows (including the first/main) 
      # user has the option to cancel the closing of modified tabs/windows
      # if 'force' is given no confirmation is asked and modified content is lost.
      # the number of schematic views  left over (in addition to main window)
      #  is returned. If only one (the main view) is left command returns 0.
      quit_xschem [force]

      raise_dialog
      read_data
      read_data_nonewline
      read_data_window
      reconfigure_layers_button
      reconfigure_layers_menu
      rectorder
      redef_puts

      # Given an absolute path 'symbol' of a symbol/schematic remove the path prefix
      # if file is in a library directory (a $pathlist dir)
      # Example: rel_sym_path /home/schippes/share/xschem/xschem_library/devices/iopin.sym
      #          devices/iopin.sym
      rel_sym_path symbol
      
      reroute_inst
      reroute_net
      reset_colors
      restore_ctx
      return_release
      rotation
      save_ctx
      save_file_dialog
      save_sim_defaults
      schpins_to_sympins
      select_inst
      select_layers
      set_bindings
      set_env
      set_graph_linewidth
      set_initial_dirs
      set_missing_colors_to_black

      # set 'var' with '$val' if 'var' not existing
      set_ne var val

      # set_netlist_dir force [path]
      # if path is given set as new netlist path where netlists and simulations are done.
      # force should be always set to 1 unless you just want to query current path.
      # select_netlist_dir 0 will return current path (you can get with $netlist_dir as well)
      set_netlist_dir

      set_old_tk_fonts

      # when XSCHEM_LIBRARY_PATH is changed this function is called 
      # by 'trace_set_paths' refresh and cache new library search paths.
      set_paths
      
      set_replace_key_binding

      # Initialize the tcl sim array variable (if not already set) 
      # setting up simulator / wave viewer commands
      set_sim_defaults

      set_tab_names
      setglob
      setup_recent_menu
      setup_tabbed_interface
      setup_tcp_bespice
      setup_tcp_gaw
      setup_tcp_xschem
      setup_toolbar
      sframe

      # show ERC (electrical rule check) dialog box
      show_infotext

      simconf
      simconf_add
      simconf_reset
      simconf_saveconf
      sim_is_ngspice
      sim_is_xyce
      sim_is_Xyce
      simulate
      simulate_button
      simuldir
      source_user_tcl_files
      sub_find_file
      sub_match_file
      swap_compare_schematics
      swap_tabs

      # show a dialog box asking user to switch undo bguffer from memory to disk
      switch_undo

      # evaluate a tcl command from GUI
      tclcmd

      tclcmd_ok_button
      tclpropeval
      tclpropeval2
      text_line
      textwindow
      to_eng
      tolist
      toolbar_add
      toolbar_hide
      toolbar_show

      # this function executes whenever XSCHEM_LIBRARY_PATH changes (registered
      # with a 'trace' command)
      trace_set_paths

      try_download_url
      update_div
      update_graph_node
      update_recent_file
      update_schematic_header
      view_current_sim_output
      waves
      write_data
      write_recent_file
      xschem_getdata
      xschem_server

 </pre>

 <h1>SOME USEFUL SCRIPT <a id="scripts">EXAMPLES</a></h1><br>


 <p> The following examples show the xschem commands one by one. In general you should create small TCL procedures 
  to perform these tasks. This way you can optimize things, for example creating temporary variables holding the
  output of the various <kbd>xschem ...</kbd> commands.</p>


 <ul>


 <li> <h3>Instantiate a component and wire it up with specific nets on its terminals.</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># Create a 5V Vvdd voltage source
xschem instance vsource.sym 100 100 0 0 {name=Vvdd value=5}</pre>
     </td></tr>
 <tr><td><img src="developer_info_08.png"></td></tr>

 <tr><td>
        <pre class="code"># Attach labels, They will get the symbol pin labels
xschem select instance vvdd
xschem attach_labels
</pre> </td></tr>
<tr><td><img src="developer_info_09.png"></td></tr>

 <tr><td>
        <pre class="code"># Select labels, unselect vsource and change positive and negative terminal
# labels to VCC and GND respectively
# The first item in the selected_set list is the first vsource terminal
# (the positive terminal), the second one is the negative terminal.
# At the end unselect all
xschem connected_nets
xschem select instance Vvdd clear
xschem setprop instance [lindex [xschem selected_set] 0] lab VCC
xschem setprop instance [lindex [xschem selected_set] 1] lab GND
xschem unselect_all
</pre></td></tr>
     <tr><td><img src="developer_info_10.png"></td></tr>
 </table><br>


 <li> <h3>Disable a component in the schematic</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># Add spice_ignore=true attribute
# the component will be ignored in generated netlists.
xschem setprop instance Vvdd spice_ignore true
</pre>
     </td></tr>
     <tr><td><img src="developer_info_11.png"></td></tr>
 </table><br>


 <li> <h3>Delete a component together with its attached nets</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># select component, select attached nets and delete
# this will also select wire segments if labels are attached to selected instance with wires.
xschem select instance Vvdd
xschem connected_nets
</pre>
     </td></tr>
     <tr><td><img src="developer_info_12.png"></td></tr>

 <tr><td>
        <pre class="code"># Delete selection
xschem delete
</pre>
     </td></tr>
     <tr><td><img src="developer_info_13.png"></td></tr>
 </table><br>


 <li> <h3>Delete dangling nets and labels</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># If after some editing or deletions dangling nets are present
# they can all be selected. Deletion may be done with a "xschem delete" command.
xschem select_dangling_nets
</pre>
     </td></tr>
     <tr><td><img src="developer_info_14.png"></td></tr>
 </table><br>


 <li> <h3>Change attributes of a group of components</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># From this situation we want to select all MOS elements with L=2
# and modify L (gate length) to 3
</pre>
     </td></tr>
     <tr><td><img src="developer_info_15.png"></td></tr>

 <tr><td>
        <pre class="code"># Do an exact search of elements with L=2
xschem search exact 1 L 2
# a more precise search to avoid selecting unwanted elements might be:
# xschem search regex 1 propstring "L=2\[ \n\].*model=nfet"
# the above command will do a regular expression search on the whole
# instance property string (the special token propstring)
foreach i [xschem selected_set] { xschem setprop instance $i L 3}
xschem unselect_all
</pre>
     </td></tr>
     <tr><td><img src="developer_info_16.png"></td></tr>
 </table><br>


 <li> <h3>Copy a components with its wired terminals</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># From this situation we want to copy Vvdd to a different location
# and change the instance name, voltage value  and its positive terminal net name
</pre>
     </td></tr>
     <tr><td><img src="developer_info_17.png"></td></tr>

 <tr><td>  
        <pre class="code"># select the desired instance
xschem select instance Vvdd
# select attached wires
xschem connected_nets
# Copy to clipboard
xschem copy
# Paste selection 150 x-axis units to the right
xschem paste 150 0
# First selected_set item is the voltage source (it was selected first)
xschem setprop instance [lindex [xschem selected_set] 0] name Vvpp
xschem setprop instance [lindex [xschem selected_set] 0] value 12
# Following item is the net label attached to the first symbol pin
xschem setprop instance [lindex [xschem selected_set] 1] lab VPP 
</pre>
     </td></tr>
     <tr><td><img src="developer_info_18.png"></td></tr>
 </table><br>


 <li> <h3>Transform a component into a short</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># We want to transform this voltage source into a short, passing the 
# negative label onto the positive terminal.
# Warning: no net label must be present on the positive net, otherwise you end up with 
# an ERC error (multiple differnet labels on the same net)
</pre>
     </td></tr>
     <tr><td><img src="developer_info_19.png"></td></tr>

 <tr><td>  
        <pre class="code"># add spice_ignore=short attribute to instance
# All pins of the instance will be shorted together to the same net.
# Instance will be shown in red to indicate the short condition.
# Option "Options-&gt;Show net name on symbol pins" is enabled and attribute 
# <kbd>net_name=true</kbd> is set on the resistor to show net names.
# you see the left resistor terminal is GND now.

xschem setprop instance Vvdd spice_ignore short
</pre>
     </td></tr>
     <tr><td><img src="developer_info_20.png"></td></tr>
 </table><br>


 <li> <h3>Move a selected portion of the schematic</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># After selecting some objects...
</pre>
     </td></tr>
     <tr><td><img src="developer_info_21.png"></td></tr>

 <tr><td>
        <pre class="code"># ... We move them by some X / Y quantities.
xschem move_objects 100 0
</pre>
     </td></tr>
     <tr><td><img src="developer_info_22.png"></td></tr>
 </table><br>


 <li> <h3>Rotate a selected portion of the schematic</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># After selecting some objects ...
</pre>
     </td></tr>
     <tr><td><img src="developer_info_23.png"></td></tr>

 <tr><td>
        <pre class="code"># ... We rotate them clockwise around point 1100,-800 (shown with the red cross)
xschem rotate 1100 -800
</pre>
     </td></tr>
     <tr><td><img src="developer_info_24.png"></td></tr>
 </table><br>


 <li> <h3>Flip a selected portion of the schematic</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># After selecting some objects as before ...
# ... We flip them horizontally around point 1100,-800 (shown with the red cross)
xschem flip 1100 -800
</pre>
     </td></tr>
     <tr><td><img src="developer_info_25.png"></td></tr>
 </table><br>


 <li> <h3>Rotate in place a selected portion of the schematic</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># After selecting some objects ...
</pre>
     </td></tr>
     <tr><td><img src="developer_info_26.png"></td></tr>

 <tr><td>
        <pre class="code"># ... We rotate clockwise each object around their origins
# the same command 'flip_in_place' is available for flipping horizontally.
xschem rotate_in_place
</pre>
     </td></tr>
     <tr><td><img src="developer_info_27.png"></td></tr>
 </table><br>


 <li> <h3>Move a wired object</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># After selecting some objects ...
</pre>
     </td></tr>
     <tr><td><img src="developer_info_28.png"></td></tr>

 <tr><td>
        <pre class="code"># ... we select only the first segments attached to their pins ...
xschem connected_nets 2
</pre>
     </td></tr>
     <tr><td><img src="developer_info_29.png"></td></tr>

 <tr><td>
        <pre class="code"># ... And then move the selection.
xschem move_objects 100 0
</pre>
     </td></tr>
     <tr><td><img src="developer_info_30.png"></td></tr>

 </table><br>


 <li> <h3>Add and wire parallel devices</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># Given this instance ...
</pre>
     </td></tr>
     <tr><td><img src="developer_info_31.png"></td></tr>

 <tr><td>
        <pre class="code"># ... The following commands will copy-paste the object and move it 
# using the "connect by kissing" feature: when separating connected
#  instances a wire is added.
xschem select instance Q1
xschem copy
xschem paste 0 0
xschem move_objects 120 0 kissing
xschem unselect_all
</pre>
     </td></tr>
     <tr><td><img src="developer_info_32.png"></td></tr>
 </table><br>


 <li> <h3>Replace symbols</h3><br></li>
 <table style="width:95%;">
 <tr><td>
        <pre class="code"># In the following schematic we want to replace the nfet3/pfet3 with nfet and pfet
# that have the bulk connection pin.
</pre>
     </td></tr>
     <tr><td><img src="developer_info_33.png"></td></tr>

 <tr><td>
        <pre class="code">
# select all instances that match "fet_01v8" model name
xschem search regex 1 model {fet_01v8}
set f {}
foreach i [xschem selected_set] {
  # Replace fet3 with fet in symbol reference
  set newname [regsub {fet3} [xschem getprop instance $i cell::name] {fet}]
  xschem replace_symbol $i $newname $f
  # remove body attribute since it is now assigned to the bulk pin
  xschem setprop instance $i body fast
  # the f parameter is for optimzing (avoid pushing undo at each iteration)
  set f fast
}
xschem unselect_all
xschem redraw
</pre>
     </td></tr>
     <tr><td><img src="developer_info_34.png"></td></tr>
 </table><br>





 </ul>

 <!-- end of slide -->
 <div class="filler"></div>
</div>

<!-- frame footer -->
<iframe seamless src="xschem_footer.html"  class="footer_iframe" >
</body>
</html>

